can't add tangency relation between line and spline.. alternative?

[cmm]

In a sketch I have a line that must be tangent to one or another curve in a different sketch (the curves are tangent to each other and continuous), depending on configuration. Configurable sketch relations would be perfect for this application, but there is no such thing. I created a spline that traces over the two curves, with the intent of relating tangency between the line and the spline instead of between the line and either of the two curves, but Solidworks would not let me add this relation. Is there a better way to accomplish my goal?

Chris Montgomery
Mechanical Engineer

 

[CorBlimeyLimey]

Would this work?

1) Create two sketches, one with a line tangent on one curve, the other with a line tangent to the other curve.
2) Create separate features from each sketch.
3) Configure the part to supress/unsupress each feature as required.


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[cmm]

Thanks for you response CorBlimeyLimey. Unfortunately for me, the feature you advise making into two independent features happens to be the first and primary feature. In other words, if I go this route I will almost have two independent parts in one part file. If there is no other way, I will just create two part files.


Chris Montgomery
Mechanical Engineer

 

[CorBlimeyLimey]

Depending on the structure of your features, you could supress the first & or second features if they are unmerged bodies. They could be extruded up to a common plane, and subsequent features could be created from that same plane, indepedent of the initial bodies.

If you really want to keep it as one part without supressed features & if you know the line length, you could use the Curve through XYZ points function to create the line, but that might be more trouble than it's worth.

However, without seeing exactly what you are trying to achieve it is difficult to know if either method would work for you.


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[CorBlimeyLimey]

OK lets back up a bit ... I just placed a line tangent to a spline using SW05. What version are you using?


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[J-C]

Actually, you can control suppression of a sketch relation per configuration.

Go to "Display/Delete Relations. in the property manager, select sketch relation then select the "Configurations" menu and change it to "This Config". Then select the suppress checkbox. You can even control it from a design table.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2